3 perpendicular tubes error

[schmidtjr]

Hi,

I tried to create 3 perpendicular tubes with part design module. The tubes are modelled as "real" tubes (with wallthickness), based on simple sketches which should be padded to the required length.

start.JPG (43.93 KiB) Viewed 1161 times

This is the situation at the beginning. 3 sketches, each containing 2 circles (inner and out diameter). In the example, the tube in the middle (on Z) has a diameter of 19mm and the others have a diameter of 16mm. The tubes on X and Z are both on the same height (z-height). In the example, the center of both tubes is 16mm from 0,0.

lastWorkingState.JPG (45.76 KiB) Viewed 1161 times

This is the last state before the error (this state is attached). Z-tube was padded to some length (100mm in the example). X-tube was padded "up to face" of Z-tube.

Now the error:
If you try to pad the Y-tube (up to face of Z-tube) you get mixed behavior:
- Either it creates a pad that is not existing (only in wireframe)
- or everything is removed except for the Z-tube inner wall
- or some rendering errors on Z-tube with no Y-tube

If X and Y tubes are not on the same height, you can pad both. If you now move them to the same height (via circle position in the sketch) FreeCad crashes or hangs endlessly.


freecad stats:
OS: Windows 10 (10.0)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.23323 (Git)
Build type: Release
Branch: master
Hash: 512d5c6141aec52b6eecc67370336a28fde862a6
Python version: 3.8.6
Qt version: 5.12.5
Coin version: 4.0.0
OCC version: 7.4.0
Locale: English/Germany (en_DE)


P.S.: Just in case someone asks for the reasoning of modelling something this way:
- for me, that's the correct attachment of tubes. one is mitered, the other one isn't touched. By doing it in Part WB, I wasn't able to achieve this. Only thing I got was one tube mitered, the other one with a hole in it.
- By modelling the real tubes, I could extract volume of the model (for weight analysis)
- (FEM) <-- for this I found that you can set the shell thickness, so this is not a valid point I guess

[chrisb]

The problem is the line between the small tubes. "To first" doesn't work, because there are different faces involved.

SnipScreenshot-d1280b.png (20.37 KiB) Viewed 1140 times

In Part workbench, you could create the big tube from full material and cut it from both smaller tubes. Then cut one of the smaller tubes from the bigger one. And finally cut the inner part from the big tube.

Please note, that the cutter still exists after a cut operation.

[schmidtjr]

Hi

oh yes, it's the overlap of the two small tubes.
And it's not related to my tubing example. It can be reproduced with a much simpler example consisting of full material cylinders.

I'll try the part wb approach in the next days. But, it does definitely not sound "straight forward" .

Kind regards,
Martin

[chrisb]

Straight forward are the tube connectors in Part workbench.

[schmidtjr]

Hi,

Please note, that the cutter still exists after a cut operation.

This hint was worth gold. For the frequent Freecad user this is obvious, but for me not (yet).

I player around with it a little bit more.

First Idea
Based on your proposal, the vertical tube was solid, the others where tubes. Cut the solid from the smaller tubes, cut one smaller tube from the other. This won't work, you'll get something like:

tubeCutError.JPG (58.61 KiB) Viewed 1048 times

Full solids
To avoid the issue of the first idea, I was starting with solids for all tubes. And at the end, I removed the inner part of the solids:

solidTubes.JPG (59.43 KiB) Viewed 1048 times

solidTubesInner.JPG (34.26 KiB) Viewed 1048 times

This looks great. And it might be the most realistic solution in regards to manufacturing/welding. The vertical tube has no holes in it, the horizontal tubes are mitered. One is mitered only to the big vertical tube, the other one is mitered to the vertical AND the other smaller horizontal tube. One could extract mitering templates out of this (I need to figure out how), put them on tubes, cut out the tubes and weld it together.
But... It's a great amount of work for such a simple example. The history tree is huge and I fear it is not servicable after some time. In half a year I won't know why it looks how it looks.

Connect objects
Still in part design, connecting the tubes with "Connect objects". Results in:

tubesConnect.JPG (57.32 KiB) Viewed 1048 times

tubesConnectInner.JPG (55.23 KiB) Viewed 1048 times

I would say, this is the fastest approach after the "part Design Workbench" approach, which seems a little bit fater. But. It creates a shape that's technically wrong (from MY merspective, not generally). The vertical tube has cut holes into it. That's not how such connections are normally manufactured.
I tried this one already some days ago, at that time it crashed after 5 tube connections or so. But now it was working, don't know why. Maybe I had too much mirroring or try and error in the last approach.

solid bodies and using "thickness"
One last approach was to create the tubes as solid objects again (all). Cut them as desired and now apply a thickness to the result. But... This looks the same as when using "connect objects".


So, I guess now it's up to me to figure out how to model it the best way. So I'm back at my start (https://forum.freecadweb.org/viewtopic.php?f=3&t=53964) still don't know how to model such a weld structure "the best" way. I need to:
- extract dimensions for manufacturing
- extract mitering tempates for manufacturing
- perform FEM analysis
- get a good estimate on the expecte weight
I don't care about modelling the actual weld joints as fillets or so. Fastest approach would be using only solids (an applying thickness at FEM, haven't checked this yet). But this would not allow weight/volume calculation.

I'll play around a little bit more.
Kind regards,
Martin